Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web
FEM/ANSYS

## S5 3D Beam Structure

Structural #5: Analysis of a 3-D Beam structure

Introduction: In this example you will learn to use the 3-D Beam element in ANSYS.

Physical Problem: Structural analysis of the bicycle frame made of hollow aluminum tubing shown in the figure.

Problem Description:

The cycle frame is made up of hollow aluminum tubing. These members can be modeled as 3D Beams. 3D beams experience bending in two directions perpendicular to the length of the beam.

Units: Use SI units only

Geometry: The tubing has an outer diameter of 25mm and a wall thickness of 2mm.

Material: Assume the structure is made of aluminum with modulus of elasticity E=75 GPa.

Boundary conditions: The structure is constrained in the X, Y and Z directions at the bottom three corners.

Objective:
 To determine deflection at each joint. To determine the maximum stress. Now assume that your friend needs a ride home and she (he) sits on the back seat (point 5). Determine the maximum stress now. Remember the extra loading depends on the weight of your friend. :)

You are required to hand in print outs for the above.

IMPORTANT NOTE: You can use the stress list to determine the maximum stress but please do not print this list. The easy way to determine the maximum stress is to take guesses where the maximum stress should be, Zoom to those points to get the node numbers or element numbers, then look for SMAX values at those nodes/elements.

Figure:

STARTING ANSYS

 Click on ANSYS 6.1 in the programs menu Select Interactive. The following menu that comes up. Enter the working directory. All your files will be stored in this directory. Also enter 64 for Total Workspace and 32 for Database. Click on Run.

MODELING THE STRUCTURE

 Go to ANSYS Utility Menu. Click on Workplane>Change Active CS to..>Global Cartesian Go to the ANSYS Main Menu Preprocessor>Modeling>Create>Keypoints>In active CS The following window comes up:

 Fill in the keypoint number (1,2,3...) and the coordinates. Make sure you get the correct coordinates from the figure. Create all the 8 keypoints. Make sure the numbering of your keypoints matches the numbering of the joints in the figure. If you cannot see the complete figure then go to Utility Menu>PlotCntrls>Pan Zoom Rotate and zoom out to see the entire figure. Now create lines connecting the keypoints Click on Preprocessor>Modeling>Create>Lines>Lines>In Active Coord Create lines by connecting keypoints.  Click OK when all of the lines are made

 You can use the Utility Menu>PlotCtrls>Pan, Zoom, Rotate window to rotate the model and see its 3D nature.

MATERIAL PROPERTIES

 Go to the ANSYS Main Menu Click Preprocessor>Material Props>Material Models.  In the window that comes up, select Structural>Linear>Elastic>Isotropic.

 The following window comes up for Material Model Number 1

 Fill in 7.5e10 for the Young's modulus and 0.3 for minor Poisson's Ratio. Click OK Now the material 1 has the properties defined in the above table. We will use this material for the structure.

ELEMENT PROPERTIES:

SELECTING ELEMENT TYPE

 Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Add... The following window opens.

 Type 1 in the Element type reference number. Click on Structural Beam and select 3D elastic. Click OK. Close the 'Element types' window So now we have selected Element type 1 to be a structural Beam 3D elastic element. The tubings will be modeled as elements of type 1, i.e. structural 3D Beam element. This finishes the selection of element type. Now we need to define the cross sectional area for this element. Go to Preprocessor>Real Constants>Add/Edit/Delete… In the "Real Constants" dialog box that comes up click on Add. In the "Element Type for Real Constants" that comes up click OK. The following window comes up.

 Fill in the relevant values and click on OK. We have now defined the cross sectional area, area moment of inertia etc. of the 3D beam element.

MESHING:

DIVIDING THE FRAME INTO ELEMENTS:
 Go to Preprocessor>Meshing>Size Controls>Manual Size>Lines>All Lines. In the menu that comes up type 0.01 in the field for 'Element edge length'.

 Now we have defined each element to be of size 10 mm i.e. 0.01 meter Click on OK. Now go to Preprocessor>Meshing>Mesh>Lines. Select all the lines and click on OK in the "Mesh Lines" dialog box. Now each line is divided into 3D beam elements.

BOUNDARY CONDITIONS AND CONSTRAINTS:

APPLYING BOUNDARY CONDITIONS
 The cycle is constrained in all DOFs at the point 3,4,6,7,8. Go to Main Menu. Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Keypoints. Select each keypoint on which you want to apply displacement constraints. The following window comes up.

 Select All DOF and click OK.

APPLYING FORCES
 Go to Main Menu Preprocessor>Loads>Define Loads>Apply>Structural>Forces/Moment>On Keypoints. Select the keypoint where the force acts. Here we use keypoints because there are a lot of nodes and therefore, it is easier to pick keypoints. Click on OK in the "Apply F/M on Keypoints" window. The following window will appear: Enter the value of the force in the Y direction. Repeat the procedure to apply the force on the other keypoint.

 The model should look like the one below:

 Now the Modeling of the problem is done.

SOLUTION:

 Go to ANSYS Main Menu>Solution>Analysis Type>New Analysis. Select static and click on OK. Go to Solution>Solve>Current LS. Wait for ANSYS to solve the problem. Click on OK and close the 'Information' window.

POST-PROCESSING:

 Listing the results: Go to ANSYS Main Menu General Postprocessing>List Results>Nodal Solution. The following window will come up.

 Select DOF solution and All U's. Click on OK. The nodal displacements will be listed as follows.  Note that the node number may not be the same node on your project depending on the order in which you picked your lines to be made.

 Similarly you can list the stresses for each element by clicking General Postprocessing>List Results>Element Solution. Now select LineElem Results. The following table will be listed.

 IMPORTANT NOTE: You can use this list to determine the maximum stress but please do not print this list. The easy way to determine the maximum stress is to take guesses where the maximum stress should be, Zoom to those points to get the node numbers or element numbers, then look for SMAX values at those nodes/elements.

MODIFICATIONS:

 You can also plot the displacements and stress. Go to General Postprocessing>Plot Results>Contour Plot>Element Solution. The following window will come up.

 Select a stress to be plotted and click OK.  The output will be like this.